[cagesbuild]

Hi all. I am trying to replicate an academic paper an circulation control. In this paper a semi-elliptical airfoil has tangential blowing on a circular trailing edge of about 80 [m/s]. This is then subjected to a free stream of about 40 [m/s]. I am using k-w SST with curvature correction with all turbulence parameters (including inlets) left at the default values and the reference area set to 8.6 [in] (chord length in the paper). Unfortunately the solver gives a "floating point exception" error. The error seems to resolve itself when set to a lower free-stream value (5[m/s]) but stops converging and becomes unstable.

I am not really sure how to fix this any help would be appreciated.
Flow Field:
flow field.jpg
Airfoil Geometry:
airofil.jpg
Tangential Blowing Injector:
Injector.jpg
(Notice the edges of the injector have a 45[deg] chamfer to overcome floating point)

[vinerm]

Could you provide more details about the material properties and solver setup?

[cagesbuild]

Sure! Although I'm not sure specifically what you require I will attempt to the best of my capabilities

Material - Air (default values)

Model - k-w SST with curvature correction enabled (default values)

Boundary Conditions -
Two Velocity inlets, one in the free stream with velocity of 39.5[m/s] directed in the x direction. Another Velocity inlet on the upper portion of the trailing edge (Shown in the "Injector" picture the left most vertical line).
One pressure outlet, the farthest right vertical line
All other lines are walls

Reference Values- Calculated from the inlet condition with reference area set to .2185[m^2]

Methods - Coupled all terms set to second order upwind, Pseudo-Transient and Higher order term relaxation enabled

Monitors- Residuals - Set to 1e-6 for all values

Initialization - I have tried Hybrid and Standard (using both the inlet and injector as the reference values

[vinerm]

Though the Mach number appears to be below 0.3, however, it is quite close to being compressible. In my view, you should use ideal gas for such velocities. Secondly, use fmg-initialization. Furthermore, I could not understand why you have a mesh outside the oval region. A better option would have been to extend this region slightly downstream and then use far-field condition instead of a square region around the airfoil. Furthermore, length of downstream domain appears to be adequate but you have too much length on the upstream. The top and bottom walls should be set to free slip, assuming those are not real walls.

[cagesbuild]

Thank you vinerm for the timely reply. I've had some time to look into your suggestions, I have removed the square region but some meshing problems gave me difficulty in fixing the other problems mentioned. Additionally a quick geometry change fixed the floating point exception, unfortunately the solver is not converging.

Changes:
Geometry:
I originally had two camfers on either side of the injector. To fix this I deleted the bottom most camfer and moved the jet face to be flush with the wall.

Initialization:
fmg-initialization: set to all defaults

Problems:
The residuals decrease rapidly then increase and "stabilize" at the same value they started at. Cl, Cd also vary substantially.

[vinerm]

Which solver are you using? Prefer Coupled Pseudo-Transient and use low factor for time-scale. Default would be 1, reduce it to 0.1 and increase it slowly, say every 100 iterations or so. You can do this via journal.

Secondly, use first-order discretization for all fields for first 500 iterations or so. Then switch to second order.

If the residuals still stall, you can try changing the gradient limiter to cell-to-cell from the default one. This can be done under Solution Controls > Advanced.

[cagesbuild]

I was using pseudo-transient for initial convergence then switching it off because it provided quicker convergence. Anyway, I was doing a last check of my values and found that my y+ values were ~20 at the maximum and ~8 on the locations of interest, which is unacceptable for the k-w turbulence model. After I decreased the y+ value, so that it was <1 everywhere, the instability cropped up again. While using all Discretizations set to first-order upwind (Pressure was set to standard) and the Coupled Pseudo-Transient scheme enabled (using both the aggressive and conservative time steps with both high and low time scales). The residuals initially decrease and then blowup again.

Is this an issue with the geometry or the meshing method perhaps? Or is this error relatively common and I just have to play around with the settings until it converges?

[vinerm]

should always be greater than 1. Making it smaller than 1 is an overkill and not useful. of 8 is not bad for . Keep it pseudo-transient and time-scale factor of 0.1. Do not disable pseudo-transient or coupled. If you use coupled but without pseudo-transient, ensure that Courant number (under solver controls) is set below 100. Default is 200. After removing the square domain, it is possible that the downstream length is not enough for the simulation to converge, however, you should see a lot of flow reversal at the outlet in that case. If it is not there, then domain length is not an issue. For pressure, use PRESTO instead of standard. Are you using constant density of air or ideal gas?

[cagesbuild]

Ahhh, that is different than most of what I have read. Is a good y+ then roughly below 10?

I had assumed Ideal gas and constant density in the initial run, and the run in the background at the time of writing. While I was playing around with some of the settings I noticed that the density based solver, in the general tab, did not diverge at all but also did not converge below 1e-6. Other than the speed of pressure based and the low mach number the current simulation is running at, is there a reason to not use the density solver?

I will update you as I try your suggestions, once again thank you for your quick response!